Duplicate Catpart with external links

[PBPouw]

I have a Catpart in an assembly with external links.
Now I want to copy / duplicate this part to create a same part with the same links but lets say 10 inch to the left.
For example a airplane metal rib, I have created rib no 1 with external links to outside surface of the wing. Now I want to make rib no 2 without having to do exactly the same as I did with rib no 1.

 

[Azrael]

Without any possibility to test I would say, copy paste/break link and relink the new one OR crete a powercopy of the rib and insert a new empty part and use the power copy OR create a part template.

 

[ferdo]

Is it EXACTLY the same CATPart? Why don't you use Assembly Workbench?

Regards
Fernando

 

[jackk]

what you want to do is called "morphing"

Copy the old rib part (use FILE + SAVE AS) to create the new rib part. Then move the rib sketch support plane 10" to the left. The new rib should "morph" based on the wing surface at the new position.

A common technique used for this is called "skeleton" where a "skeleton" part is created with all the planes (such as Rib centerplanes) and surfaces. These planes and surfaces are copied with links to the appropriate individual parts. As the airplane is developed, these surfaces and planes can be adjusted in the "skeleton" resulting in all the linked parts adjusting accordingly.

 

[ferdo]

Jackk is right, you can see an example here

http://www.youtube.com/watch?v=NeOv9w4WoLY

and is good to read also

http://www.catiav5forum.de/wbb3/wbb/index.php?page=Thread&threadID=6444

Regards
Fernando

 

[PBPouw]

The Youtube exactly shows how not to do it !

Look at time 5.11 Catia gives the following warning :

The reference of the component Rib2.1
is a new version of a contexed component
to be able to edit it yo must
-either isolate it
-either define its new context

Further look in the external references of rib 2, they are all broken and no longer connected to the original wing surface.

Azrael is right that you can reconnect the links but for example in the youtube clip there are only 3 references.
I have catparts with more then 50 links. I find it a waist of time to reconnect them.

 

[Azrael]

If you create a template part and use meta data instantiation you can pick all 50 references with one click if they are published.

 

[PBPouw]

Azreal,

can you explain a little further how do I use metadata instantiaton ( couldn't find it on the web ) and where can I find it in Catia.

I already had the thought that you need published elements.

 

[ferdo]

That's funny, you are right, in the video its look to be isolated but they linked, see the photo. And is true that you have to open in a new window to modify the position of the plane (define its new context).

http://i198.photobucket.com/albums/aa175/kotra30/2009-11-23_113626.png

Regards
Fernando

 

[Azrael]

Chech the documentation, PKT workbench, should be in the chapter about Part and Assembly templates, look for "meta input".

When you create a part template is will identify the external links and use them as input, you can also add additional inputs. In the template window there is a tab called meta inputs where you can define that a certain string corresponds to a set o parameter, note that the naming of the parameters from the input tab have to correspond to the published named the parts use in the context you want to instantiate it in. Group the meta inputs so the correspond to the different parts you need to use when instantiating. I.e if you have one part with 10 elements you want to link to and another part with 15 elements then you need to set up two sets when creating the template with corresponding parameters.

Very powerful if you have a controlled enviroment

 

[PBPouw]

Thanks Azreal,

Think I have to put my nose in the study books.

This is completely new material to me.